Post Go back to editing

Photodiode Wizard and the SPICE model it generates give very different noise levels

I realize the photodiode wizard is approximate while SPICE is a little more rigorous, but the difference for this circuit is very large:

A low level of noise is estimated:

If I download the spice file for that circuit and run it in ltspice, then integrate noise over the target bandwidth, I get:

SPICE predicts 3x worse noise, and furthermore, SPICE is assuming a brickwall filter at 30 MHz, so real performance would be worse.  Am I doing something wrong in SPICE or is the photodiode wizard just really inaccurate?

  • Hi mgiacomelli, 

    I am looking into this. Could you send me the design files you generated from the Photodiode Wizard? I would like to see the parameters of your circuit. 



  • Unfortunately the wizard deleted my design before I could save it, but I was able to type them back in from the SPICE file:

    	"Name": "for forums",
    	"Description": "ddd",
    	"Tool": "PD",
    	"Design": {
    		"photodiode": {
    			"sensor": "",
    			"reverseVoltage": "50",
    			"biasPreference": "positive",
    			"capacitance": "3.5e-10",
    			"shuntResistance": 1000000000,
    			"peakCurrent": "0.001",
    			"peakVoltage": "1",
    			"speedPreference": "bandwidth",
    			"speed": "30000000",
    			"peaking": 0.707107,
    			"stages": "1",
    			"opAmps": [
    					"stage": "stage_1",
    					"opAmp": "ADA4895-1",
    					"locked": false,
    					"found": true,
    					"valid": true
    	"CreatedDate": "2018-09-04 05:04:55 PM",
    	"UpdatedDate": "2018-09-04 05:04:55 PM"

  • mgiacomelli,

    My apologies for the delayed reply.  Also, thank you for the screen shots and the design files information - it was very helpful in troubleshooting this issue.

    It is usually the case that the results from the SPICE schematic generated by Photodiode Wizard will closely match the results reported in Photodiode Wizard.  The mismatch in noise results between LTspice and Photodiode Wizard was not a result of you doing anything wrong.  Thank you for bringing this mismatch to our attention.

    I've investigated this issue, and have determined that the SPICE model for this device (ADA4895) does not accurately model noise at higher frequencies ( greater than 3MHz ).  I've also investigated the noise results from Photodiode Wizard, and I do believe those results are accurate.

    If you'd like to verify the Photodiode Wizard calculations by hand, you can compare the Spectral Noise plot in the Photodiode Wizard to the calculations on page 21 of the ADA4895 datasheet.  You can also refer to High Impedance Sensors for more information about the calculations.


  • Thanks.

    From those equations,

    f2 = 1/(2*pi*1000*9.1E-12) = 1.7490e+07

    f3 = 1.E9*9.1E-12/350E-12 = 2.6000e+07

    Output voltage noise  =  1E-9*(350E-12/9.1E-12)*sqrt(2.6000e+07*1.57) = 2.4573e-04 V which is in good agreement with the photodiode wizard.  I am surprised that the spice model for a 1 GHz opamp doesn't work above 3 MHz however.  Is the spice model linked on the analog product page any better?

  • mgiacomelli,

    I'm glad you were able to verify the results from Photodiode Wizard using the formulas in the datasheet.

    I've checked the SPICE model on the product page, and it has the same issue as the model in LTspice.

    We are working on a fix for this issue - I will follow-up on this thread when an updated model is available.